CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   RasInterFoam STRANGE RESULTS AT BOUNDARY (http://www.cfd-online.com/Forums/openfoam-solving/59013-rasinterfoam-strange-results-boundary.html)

kumar2 March 22, 2006 19:32

Hello friends I have been u
 
Hello friends

I have been using rasInterFoam to study wave making of hydrofoils in a channel. the problem i am experiancing is that although i have defined an outlet the fluid seems to be flowing back into the computational domain . let me explain this in detail. figure 1 shows the boundary conditions i have imposed
http://www.cfd-online.com/OpenFOAM_D...your_image.gif

The boundary conditions for the atmosphere are exactly same as that of damBreak case in rasInterFoam tutorial. The boundaries for hydrofoil is simple ( basically a noslip wall)

http://www.cfd-online.com/OpenFOAM_D...your_image.gif
http://www.cfd-online.com/OpenFOAM_D...your_image.gif
http://www.cfd-online.com/OpenFOAM_D...your_image.gif
http://www.cfd-online.com/OpenFOAM_D...your_image.gif

figure 2, 3 , 4 & 5 shows the results after only 1000 time steps . As you can see there seems to be a serious error at the outlet. The velocity seems to have significantly slowed down and the flow seems to change direction and flow back into the domain ( see for example figure 5). i wonder what is happening to the mass conservation equations?

Could anyone please comment on these results

Thanks in advance
kumar

hjasak March 22, 2006 20:05

Can't see the images - could y
 
Can't see the images - could you please try and upload them again?

Thanks,

Hrv

kumar2 March 22, 2006 20:12

Sorry friends my images are
 
Sorry friends

my images are too big . so could not upload. but let me explain with 2 figures. figure 1 shows gamma. you can also notice the inlet . there are 2 patches for the inlet so that gamma is 0 in the top and 1 in the bottom. U is specified and equals 0.8 in top & bottom patches . pd has zero gradient. there are also small values for k & epsilon .

http://www.cfd-online.com/OpenFOAM_D...ges/1/2020.jpg

The top boundary is atmosphere and the boundary conditions are same as in the tutorial of rasinterFoam.

The outlet is specified as two outlet patches with zero gradient for most quantities ( including U ). But gamma is 1 for the bottom patch of outlet and 0 for top patch of outlet. pd is set to zero as shown below ( in file /0/pd)
patch atmosphere
{
type totalPressure;
p0 uniform 0;
value uniform 0;
}

the hydrofoil is a noslip boundary and bottom of channel is symmetryPlane.

http://www.cfd-online.com/OpenFOAM_D...ges/1/2021.jpg

figure 2 shows the velocity field. you can see that the flow is decelerating and turning back into the computational domain . something terribly wrong is happening at the outlet

all comments welcome

thanks in advance
kumar

kumar2 March 22, 2006 20:16

Dear Hrv I would love to he
 
Dear Hrv

I would love to hear your comments . i have just uploaded the images

regards

kumar

hjasak March 22, 2006 20:42

You need to change the outlet
 
You need to change the outlet boundary condition. Definitely not totalPressure on pd - use either fixedValue zero or zeroGradient (my bet is on zeroGradient, but this kind of thing is worth trying out). On U, use zeroGradient and on gamma do inletOutlet, using some sensible distribution for the refValue.

Your problem is definitely caused by the pressure b.c.

Good luck,

Hrv

kumar2 March 22, 2006 21:42

Dear Hrv thanks a lot for y
 
Dear Hrv

thanks a lot for your comments. now that i know there is a problem with the pressure.b.c i am going to try out your suggestions. i will let you know once i fix the problem.

thanks a lot once again

regards

kumar

kumar2 May 23, 2006 18:07

Hello Dear Friends The figu
 
Hello Dear Friends

The figures show waves generated by a hydrofoil with rasInterFoam + nuTilda turb.model. The Boundary Conditions are like in the prevoius posts , as recommended by HRV. i got good results with k epsilon model . But k epsilon model has problems in the low Re range ( the Cp distribution has problems which in turn is reflected in the free surface deflections) . so i switched over to spallart allmaras model and my results are blowing up ! The free surface profile , velocity magnitude and nuTilda ( just before the solution blows up) are shown in the 3 figures. What seems to be happening is that the nuTilda gets very large near the atmosphere and the solution blows up. Please also note the patches of zero velocity near the atmosphere.

http://www.cfd-online.com/OpenFOAM_D...ges/1/2427.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/2428.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/2429.jpg

Note the hydrofoil is at the bottom left corner.

The top wall is modeled as the atmosphere with U as ( 0 0 0) - similar to the damBreak case . or should this be (0.8 0 0) ? where 0.8 is the inlet velocity
///////////////////////////////////////////
The important BC's for nuTilda are

InternalField = 5.7*10^-6 ;

1. atmosphere
type inletOutlet;
inletValue uniform 5.7e-06;
value uniform 5.7e-06;

2. Both the inlets ( one for air and one for water have fixedValue nuTildas of 5.7e-06 )

//////////////////////////////////////////////
The nuTilda value that i have specified are different from those given in the rasInterFoam tutorial . I found that with those ( the tutorial case )there was severe fluctuations of the free surface profiles - because of concentrations of nuTilda near the free surface. Also the nuTildas i have specified above resemble more closely the 'k' boundary condition.


All comments are welcome.

Thanks a lot

Kumar

jack2000 March 9, 2007 16:22

Hi, Dear all, Can anybody tel
 
Hi, Dear all,
Can anybody tell me if it is possible to use pressure inlet boundary ( without giving velocities) in interFoam solver. I tested this kind of boundary in simpleFoam, it worked. When I tried to use it in interFoam Solver, if gamma=0, it worked; but when gamma=1, it would broken-up.

What I intend to use this kind of boundary is to simulate constant head of water head passing through a hump in a open channel, and study the flow passing capacities. Thus it seems I need gamma=1?

Thanks in advance!

Jack

onurdundar March 24, 2008 19:38

I am trying to solve a back st
 
I am trying to solve a back step in rasinterfoam with k epsilon turbulence model. I added boundary
conditions in FoamX but when I run the rasInterFoam
it gives error about boundary conditions. I run after making the given correction. The result is this
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/home/dundar/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"

I can not find a true boundary conditions.
fvSchemes and FvSolution is the same with damBreak
Thanks for your concern

Onur


The boundary conditions are
inleta atmosphere
inletw inlet
outlet atmospehre
lowerwall wall

############################################
U
boundaryField
{
inleta
{
type pressureInletOutletVelocity;
phi phi;
value uniform (0.4289 0 0);
}

inletw
{
type fixedValue;
value uniform (0.4289 0 0);
}

outlet
{
type pressureInletOutletVelocity;
phi phi;
value uniform (0 0 0);
}

lowerWall
{
type fixedValue;
value uniform (0 0 0);
}

atmosphere
{
type pressureInletOutletVelocity;
phi phi;
value nonuniform List<vector>
#############################################
pd
boundaryField
{
inleta
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho none;
psi none;
gamma 1;
value uniform 0;
}

inletw
{
type zeroGradient;
}

outlet
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho none;
psi none;
gamma 1;
value uniform 0;
}

lowerWall
{
type zeroGradient;
}

atmosphere
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho none;
psi none;
gamma 1;
value uniform 0;
}
##############################################
k
boundaryField
{
inleta
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

inletw
{
type fixedValue;
value uniform 0.00184;
}

outlet
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

lowerWall
{
type zeroGradient;
}

atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
##############################################
gamma
boundaryField
{
inleta
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

inletw
{
type fixedValue;
value uniform 1;
}

outlet
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

lowerWall
{
type zeroGradient;
}

atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

################################################
R
boundaryField
{
inleta
{
type inletOutlet;
inletValue uniform (0 0 0 0 0 0 0 0 0);
value uniform (0 0 0 0 0 0 0 0 0);
}

inletw
{
type fixedValue;
value uniform (0 0 0 0 0 0 0 0 0);
}

outlet
{
type inletOutlet;
inletValue uniform (0 0 0 0 0 0 0 0 0);
value uniform (0 0 0 0 0 0 0 0 0);
}

lowerWall
{
type zeroGradient;
}

atmosphere
{
type inletOutlet;
inletValue uniform (0 0 0 0 0 0 0 0 0);
value uniform (0 0 0 0 0 0 0 0 0);
}
#################################################
Epsilon
boundaryField
{
inleta
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

inletw
{
type fixedValue;
value uniform 0;
}

outlet
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

lowerWall
{
type zeroGradient;
}

atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
#################################################
nutilda
boundaryField
{
inleta
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

inletw
{
type fixedValue;
value uniform 0;
}

outlet
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

lowerWall
{
type fixedValue;
value uniform 0;
}

atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

fvSchemes and FvSolution is the same with damBreak
Thanks for your concern

Onur


All times are GMT -4. The time now is 20:16.